Solution Step dialog box (Multiphysics)

Solution
Name	Sets a name for the step.
Solver Type****Analysis Type	Display the solver type and analysis type of the parent solution.
Step	Specifies the type of step to create.Step - Nonlinear Statics — Structural solution step that supports a nonlinear statics structural solve. This type of step can also include geometry and material plasticity or creep nonlinearity.This step is available when Analysis Type is set to Structural.Step - Nonlinear Dynamics — Structural solution step that supports a nonlinear dynamics structural solve. This type of step can also include geometry and material plasticity or creep nonlinearity.This step is available when Analysis Type is set to Structural.Step - Thermal Nonlinear Statics, Step - Flow Nonlinear Statics, and Step - Thermal Flow Nonlinear Statics — Coupled solution step that combines a nonlinear statics structural solve with a thermal, flow, or thermal-flow solve, respectively. These types of steps can also include geometry and material plasticity or creep nonlinearity.These steps are available when Analysis Type is set to Coupled Thermal-Structural, Coupled Flow-Structural, or Coupled Thermal-Flow-Structural.Step - Thermal Nonlinear Dynamics, Step - Flow Nonlinear Dynamics, and Step - Thermal Flow Nonlinear Dynamics — Coupled solution step that combines a nonlinear dynamics structural solve with a thermal, flow, or thermal-flow solve, respectively.These steps are available when Analysis Type is set to Coupled Thermal-Structural, Coupled Flow-Structural, or Coupled Thermal-Flow-Structural.Step - Preload — Structural solution step that can include a bolt preload. This step should be placed before all static solution steps in which you plan to include the bolt preload.This step is not available when Analysis Type is set to Thermal, Flow, or Coupled Thermal-Flow.Step - Normal Modes — Modal solution step that can use the stiffness conditions (such as stress stiffening, follower stiffness, and spin softening) from the previous static solution step. This step should be placed after the static solution step for which you want to include the stiffness conditions.This step is not available when Analysis Type is set to Thermal, Flow, or Coupled Thermal-Flow.Step - Cyclic Modes — Structural and coupled solution step supports the cyclic symmetric solution for normal modes at higher harmonic indices. The software computes the harmonic modes about the nonlinear stress or displacement state at the end of the previous static step in the solution. It allows you to specify the harmonics for which to solve for or choose a set of harmonics using the Harmonics Set modeling object.This step is not available when Analysis Type is set to Thermal, Flow, or Coupled Thermal-Flow.Step - Axisymmetric Fourier Modes — Structural solution step in which the software computes the harmonics modes about the nonlinear stress or displacement state at the end of a previous static step in the solution.This step is available when 2D Solid Option is set to any option other than None. It is not available when Analysis Type is set to Thermal, Flow, or Coupled Thermal-Flow.Step - Thermal, Step - Flow, and Step - Thermal Flow — Thermal, flow, or thermal-flow solution step in which you define the solution type as steady-state or transient.These steps are available when Analysis Type is set to Thermal, Flow, or Coupled Thermal-Flow, respectively.For more information, see Defining multiphysics solution steps.
Steps to Create	Sets the number of steps to create.
Relative Position	Specifies the position of this step as it will appear in the Simulation Navigator relative to the other steps in this solution and the sequence in which it will be processed during the solve.
Make Active	Actives the step for editing and adding loads and constraints after it is created.

General page

Option	Description
Description	Sets an optional description for the solution step.
User Defined Text
Not available when Analysis Type is set to Thermal, Flow, or Coupled Thermal-Flow.
Case Control User Defined Text	Lets you insert text or a file in the Case Control section of the input file.Select an existing modeling object from the list or click Create Modeling Object to create a new one.Click Edit to edit the selected user defined text modeling object.
Boundary Condition Control Variables
Not available when Analysis Type is set to Thermal, Flow, or Coupled Thermal-Flow.
Evaluation Frequency	Specifies the value used to evaluate a frequency-dependent boundary condition when you use the boundary condition in a solution that does not support dependent boundary conditions.The software first uses the field evaluation value for the step to determine the loading value. If no field evaluation value is defined for the step, the software uses the field evaluation value for the solution.

Step Control page

Structural Control
Use Step Name as Label	For the structural solver, controls whether the software uses the specified name as the label for the corresponding Nastran subcase. When you export or solve your model, the software uses the specified name to write out a LABEL case control command for the associated SUBCASE case control command in the Nastran input file.
Sequential Dependency on Previous Subcase	Indicates whether this step depends on results from the previous step.By default, a solution step is sequentially dependent on the results of the previous solution step, and its start time is the End Time of the previous solution step. You can disable this dependency by setting Sequential Dependency on Previous Subcase to No. When this option is set to No, the start time of the solution step is 0.
Nonlinear Control Parameters	Lets you select a Nonlinear Control Parameters modeling object to define parameters that control the iteration strategy.Select an existing modeling object from the list or click Create Modeling Object to create a new modeling object.Click Edit to edit the selected object.For more information, see, NLCNTL.
Eigenvalue Extraction Method	Available when Step is set to Step - Normal modes, Step - Cyclic Modes or Step - Axisymmetric Fourier Modes.Lets you select the Real Eigenvalue-Lanczos modeling object for the step. You use a Real Eigenvalue-Lanczos modeling object to specify options for eigenvalue extraction, including the frequency range and the method for normalizing eigenvectors.Select an existing modeling object from the list or click Create Modeling Object to create a new eigenvalue extraction object.Click Edit to edit the selected object.For more information, see:Defining eigenvalue extraction data for Nastran analysesEIGRL in the Simcenter Nastran Quick Reference Guide.Eigenvalue Extraction Methods in the Simcenter Nastran Basic Dynamic Analysis User’s Guide.
Harmonics to Compute	Available when Step is set to Step-Cyclic Modes or Step-Axisymmetric Fourier Modes.Lets you select or create the Harmonics Set modeling object that specifies the harmonic numbers for which the software should compute a modal solution.Select an existing modeling object from the list or click Create Modeling Object to create a new Harmonics Set.For more information, see Specifying harmonic index numbers.
Thermal Control/Flow Control/Thermal Flow Control
Available when Step is set to Step - Thermal Nonlinear Statics, Step - Thermal Nonlinear Dynamics, Step - Flow Nonlinear Statics, Step - Flow Nonlinear Dynamics, Step - Thermal Flow Nonlinear Statics, Step - Thermal Flow Nonlinear Dynamics, Step - Thermal, Step - Flow, or Step - Thermal Flow.
Solution Type	Specifies whether the thermal and flow solvers will perform Transient or Steady State solutions during the analysis.A transient solution requires at least two solution steps with Solution Type set to Transient.Note: The flow solver does not support a mixture of steady-state and transient steps in the same solution.

Time Step Definition page

Time Step Control/Structural Control/Thermal Control/Flow Control/Thermal Flow Control
End Time	Sets the end time for the step. The sequence of steps is based on the End Time that you define for each step.For more information, see Controlling time steps in a coupled solution.
Time Step Option	Specifies the method to calculate the time steps.Number of IncrementsLets the solver calculate the increment size by dividing the simulation time interval by the number of increments. You set the value in the Number of Increments box. For the structural solver, the number of increments is the number of equal subdivisions of the load change defined for the step. You can define a different number of increments for the structural, thermal, and flow solvers.With Preload steps, time steps are always calculated in terms of the number of increments.Constant Step SizeLets you define a constant size for the time step. You set the value in the Step Size box. You can define a different step size for the structural, thermal, and flow solvers.AutomaticLets the solver calculate the time step size automatically based on the temperature error tolerance of the estimated error between the analytical solution and the simulation. The error is the difference between a fit quadratic function and a linear variation through three consecutively computed temperature values for two consecutive time steps. The time step is kept between the specified minimum and maximum values. You set the values in the Temperature Error Tolerance box, the Minimum Time Step box, and the Maximum Time Step box. See Adaptive time stepping method for more information.When the steps are created from customer default options and condition sequence information, maximum and minimum time step values could be invalid. For example, the minimum time step could be greater than the maximum time step or the maximum time step could be greater than the step interval. In these cases, the thermal solver adjusts the time step values automatically to make them valid and outputs a message to the log file.Note: The flow solver does not support this option.
Flow Time Integration Method	Available in the Flow Control or Thermal Flow Control group, or when Analysis Type is set to Flow.Specifies the integration method for the flow solver.ImplicitA first-order accurate temporal discretization method.Semi-implicit Second-orderResolves transient flow features with a significantly greater accuracy than the Implicit method for a given timestep size using the flow solver. This method is a second-order accurate temporal discretization method. Because LES simulations accurately capture flow structures with a wide range of associated time scales, use this method when you model flow fields using the LES turbulence model.
Output Control
Output Flag	Specifies the output time points at which the software writes the results to the results file.During the course of a coupled analysis, the structural, thermal, and flow solvers perform many solves. You may want to output data for post processing at each of these solution points or only at certain points.Requested IncrementsOutputs data at each of the time step increments for the structural, thermal, and flow solvers.Solution Step End TimeOutputs data only at the End Time for the current solution step.All Coupling TimesOutputs data only at the coupling times, which, depending on the Coupling Time Option, may be the same as requested increments.All TimesOutputs data:At all structural time steps and all coupling times for structural analysis.At all thermal time steps and all coupling times for thermal analysis.

Results Options page

Option	Description
Structural Output Requests	Specifies the output request for the structural solver at this step.Select an existing output request from the list or click Create Modeling Object to create a new output request.Click Edit to edit the selected output request.
Thermal Output Requests	Specifies the output request for the thermal solver at this step.
Flow Output Requests	Specifies the output request for the flow solver at this step.
Thermal-Flow Output Requests	Specifies the output request for the thermal-flow solver at this step.
Harmonics Output	Available if Step is set to Step - Cyclic Modes or Step-Axisymmetric Fourier Modes.Controls whether the software generates results for all harmonics numbers or only for specified harmonics numbers.
Harmonics Set	Available if Step is set to Step - Cyclic Modes or Step-Axisymmetric Fourier Modes.Lets you select or create the Harmonics Set modeling object that specifies the harmonic numbers for which the software should generate results.Select an existing modeling object from the list or click Create Modeling Object to create a new Harmonics Set.For more information, see Specifying harmonic index numbers.

Learn more

Defining multiphysics solution steps

Controlling time steps in a coupled solution

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Solution Step dialog box (Multiphysics), Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });